SIEMENS. Modeling assemblies. Self-Paced Training. spse01540

Transcription

1 SIEMENS Modeling assemblies Self-Paced Training spse01540

2 Proprietary and restricted rights notice This software and related documentation are proprietary to Siemens Product Lifecycle Management Software Inc Siemens Product Lifecycle Management Software Inc. 2 Modeling assemblies spse01540

3 Contents Proprietary and restricted rights notice Course introduction Solid Edge Assembly Placing parts in assemblies PathFinder in assemblies Understanding Assembly relationships Capture Fit command Capture the assembly relationships for a part Activity: Positioning parts with Mate, Axial Align, Planar Align and Insert Overview Create a new assembly and position the first part Applying a Mate relationship Applying a Planar Align relationship Applying an Axial Align relationship Applying a Mate relationship with Reduced steps Applying a Planar Align relationship with reduced steps Applying a Axial Align relationship with Reduced Steps Placing a fastener with the Insert command Summary Activity: Placing parts in an assembly using FlashFit Overview Place the first part in the assembly Use FlashFit to position the valve parts and subassemblies Place the remaining parts Summary Lesson review Lesson summary More Assembly Relationships Connect Relationship Activity: Positioning assembly parts using the Connect relationship Overview Open the assembly Position the lid by connecting 3 points Use spherical faces to define a connect relationship Summary Activity: Positioning assembly parts using the Angle relationship Overview Open the assembly Create a Connect relationship spse01540 Modeling assemblies 3

4 Contents Create an Axial Align relationship Position the lid using the Angle relationship Edit the angle Summary Lesson review Lesson summary The Assemble command Assemble command Activity: Using the Assemble command Overview Assemble command setup Assemble the parts beginning with the top cap Position the first fasteners on the top cap Position the other fasteners using edge selection Position the handle subassembly Summary Lesson review Lesson summary Designing in the context of an assembly Activity: Designing in the context of a Synchronous assembly Overview Open the assembly Modify the plastic part to make the brackets fit Shorten the brackets Create clearance between the bracket and plastic housing In-place activate the plastic part and create Inter-Part geometry for cutting the part Cut the plastic part using the Inter-Part faces Modify the angle of the opening in the plastic part Summary Lesson review Lesson summary Modeling assemblies spse01540

5 Lesson 1: Course introduction Welcome to Solid Edge self-paced training. This course is designed to educate you in the use of Solid Edge. The course is self-paced and contains instruction followed by activities. Start with the tutorials Self-paced training begins where tutorials end. Tutorials are the quickest way for you to become familiar with the basics of using Solid Edge. If you do not have any experience with Solid Edge, please start by working through the basic part modeling and editing tutorials before starting self-paced training. Tutorials Adobe Flash Player required for videos and simulations To watch videos and simulations, you must have the Adobe Flash Player version 10 or later installed as a plug-in to your browser. You can download the Flash Player (free) at the spse01540 Modeling assemblies 1-1

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7 Lesson 2: Solid Edge Assembly An assembly is a collection of parts and subassemblies that are positioned in a meaningful way. The parts can be in their final orientation, or have freedom of movement in translation and rotation. Solid Edge Assembly provides the tools needed to lay out and position the parts relative to each other. Many methods exist to accomplish this task and these approaches to building assemblies will be covered in this text. Objectives This lesson introduces the Solid Edge Assembly interface and discusses the different workflows for creating an assembly with the most commonly used part relationships. spse01540 Modeling assemblies 2-1

8 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Placing parts in assemblies The Insert Component command displays the Parts Library. You can place any of the following types of solid parts in Solid Edge assemblies using the Parts Library tab: A part constructed in the Solid Edge Part environment. A part constructed in the Solid Edge Sheet Metal environment. Another assembly constructed in the Solid Edge Assembly environment. Any file that is open in Solid Edge other than a draft file. The Insert Component command The Insert Component command will ensure that the parts library is shown. The parts library allows you to browse for the assembly components to place in the assembly. Placing the first part in an assembly Dragging assembly components from the Parts Library or Windows Explorer is the way to place a component into an assembly. To start the part placement process, in the Parts Library tab, select the part you want, then drag it in the assembly window. You can also start the part placement process by double-clicking the part in the Parts Library tab. The first part you place into an assembly is important. It serves as the foundation upon which the rest of the assembly will be built. Therefore, the first part should represent a fundamental component of the assembly. Because the first part is placed grounded, you should pick a part with a known location, such as a frame or base. Although Solid Edge makes it easy to edit parts during the design cycle, the first part you place in the assembly should be as completely modeled as possible. In the same way, although it is easy to delete parts from assemblies and change assembly relationships, the first part you place should remain grounded and not be deleted. To reposition the first part, you should first delete the ground relationship. You can then apply assembly relationships between the first part and the assembly reference planes or subsequent parts you place in the assembly. 2-2 Modeling assemblies spse01540

9 Solid Edge Assembly Placing additional components in an assembly Additional assembly components can be placed by dragging from the Parts Library, Assembly PathFinder, or Windows Explorer and dropping into the assembly window. You can use the Assembly tab on the Options dialog box to specify whether subsequent parts are temporarily placed in the assembly window (A), or displayed in a separate Place Part window (B). When you set the Do Not Create a New Window During Place Part option, the part is temporarily placed in the assembly window at the location where you dragged and dropped the part. To make the positioning process easier, drop the part in a location where it is easy to select the positioning elements you want to use. If you start the part placement process by double-clicking the part in the Parts Library tab, the display area of the assembly window is adjusted so you can see the new part. When you clear the Do Not Create a New Window During Place Part option, the part is displayed in a separate Place Part window. If the active window is maximized, the Place Part window is also maximized, essentially hiding the assembly window from view. Due to this, beginning users should not maximize the active window. Let the windows overlap, and this will make placing parts into the assembly and applying relationships much easier. spse01540 Modeling assemblies 2-3

10 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Positioning parts You use assembly relationships to position the new part relative to a part already in the assembly. The Relationships Types option on the Assemble command bar contains a wide range of assembly relationships for positioning parts relative to one another. In addition to traditional assembly relationships, the FlashFit option reduces the steps required to position a part using the mate, planar align, or axial align relationships. This option is recommended in most situations. For example, you can use FlashFit to mate a face on the placement part (A) with a face on the target part (B). After you apply the first assembly relationship, the new part is repositioned within the assembly. 2-4 Modeling assemblies spse01540

11 Solid Edge Assembly As you apply the remaining assembly relationships, the software positions and reorients the part in the assembly. Additional parts can be positioned relative to any part in the assembly, or even relative to more than one part in the assembly. You can also position a part relative to an assembly sketch. For more information on positioning parts using assembly relationships, see the Assembly Relationships Help topic. Note By default, Solid Edge maintains the relationships with which you position the part. If you clear the Maintain Relationships command on the Parts Library shortcut menu, the relationships will be used only for positioning, and the part will be grounded. Grounded parts do not update their positions when you make design changes. spse01540 Modeling assemblies 2-5

12 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Placing parts that are not fully positioned It is a good idea to fully position parts as you place them into assemblies. Fully-positioned parts will update their positions more predictably when changes are made. At times, though, you may want to place a part without fully positioning it. For example, you may be placing another part later that will be used to complete the positioning of both parts. You can use the Esc key to interrupt the placement sequence at any time. If no relationships have been applied, the part is placed in the assembly at the same relative position it occupies in the part document. In other words, the part is placed in the assembly such that the base reference planes in the part document (A) are coincident with the base reference planes in the assembly (B). If you work with the Do Not Create a New Window During Place Part option set, the part is placed in the assembly at the location you dragged and dropped it into the assembly. If you work with the Do Not Create a New Window During Place Part option cleared, the part is placed in the assembly such that the base reference planes in the part document (A) are coincident with the base reference planes in the assembly (B). You can also interrupt the placement process by selecting another command, for example, the Select tool. 2-6 Modeling assemblies spse01540

13 Solid Edge Assembly Placing the same part more than once If you want to place the same part in an assembly more than once, you do not have to use the Parts Library tab every time. After you place the part the first time, you can select it, copy it to the Clipboard, and then paste it into the assembly. When you select the Paste command, the part is displayed in a separate window, as if you had selected it from the Parts Library tab. You can then apply assembly relationships between the new part and the other parts in the assembly. You can also use PathFinder to place an existing part into an assembly again. Select the part in PathFinder, then drag and drop it into the assembly window. If a part is being placed in the assembly several times using the same relationship scheme, you can use the Capture Fit command to store the relationships and faces used to position the part the first time. This reduces the number of steps required to define each relationship when you place the part again. When you place the part later, you do not need to define which relationship and face you want to use on the placement part. You only need to select a face on the target part in the assembly for each relationship. Positioning a set of parts You can use the Assemble command to position a set of parts relative to each other without fully constraining each part in an ordered sequence. This type of workflow can make it easier to position a set of interrelated parts, such as when building a mechanism. First, drag and drop the set of parts into the assembly. Then click the Assemble command and apply relationships between one part and the other parts. To position a different part, click the right mouse button. Finding parts If you do not know the name and location of a part or subassembly, you can define search criteria using Search button on the Parts Library tab. You can then double-click the name of the part or subassembly from the list of search results to start the part placement process. spse01540 Modeling assemblies 2-7

14 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Part placement properties When you place a part or subassembly into an assembly, Solid Edge sets properties that determine the following: The placement name of a part or subassembly. Whether the part is selectable or not selectable. The quantity of the part. The x, y, and z location for grounded parts or parts or not positioned using assembly relationships. Whether the part is displayed in a higher level assembly. Whether the part is displayed in a drawing of the assembly. Whether the part is considered a reference part in a drawing or parts list. Whether the part is used in a report, such as a Bill of Material. Whether the part is used in mass property calculations of the assembly. Whether a part is used in an interference analysis calculation. You can also change these properties later using the Occurrence Properties button on the Place Part command bar or the Occurrence Properties command when selecting assembly components. Placing simplified parts The Use Simplified Parts command on the Parts Library shortcut menu allows you to specify whether you want to use the simplified or designed version of a part when placing it in the assembly. When you have the Use Simplified Parts command set (there is a check mark adjacent to the command), any faces that were deleted when simplifying the part will not be available for positioning purposes. To make these faces available, clear the Use Simplified Parts command. 2-8 Modeling assemblies spse01540

15 Solid Edge Assembly Placing subassemblies You can place a Solid Edge assembly document into another assembly in much the same way you place an individual part. When placing an assembly, in the Place Part window, you must first select the placement part in the assembly you want to use for positioning purposes, then the face on the part. If you are placing a large subassembly, you can save a display configuration in the subassembly first, then use this configuration to make placement easier. For example, you can hide all the parts, except those that will be used to position the subassembly. Before you place the subassembly, make sure the Use Configuration command on the shortcut menu is set. Then, when you place the subassembly, you can select the configuration name from the Configuration list on the Use Configuration dialog box. Subassemblies also place faster if parts have been hidden. When placing a subassembly using FlashFit or the Reduced Steps mode, the placement part step is skipped. You specify the placement part by selecting a face on the placement part you want. The placement part must be active before you can select a face. If the placement part is not already active, you can use the Activate Part button on the Place Part command bar to activate the placement part. Note When placing parts into a subassembly, you can set an option that controls whether the part is displayed in higher level assemblies. If the Display When Assembly Is Attached As Subassembly option on the Properties dialog box is cleared for a part, that part will not be displayed in PathFinder or the graphics window in higher level assemblies. spse01540 Modeling assemblies 2-9

16 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly PathFinder in assemblies The PathFinder tab helps you work with the components that make up your assembly. It provides alternate ways to view the composition and arrangement of the assembly, besides looking at the graphics in a regular assembly window. You can also use PathFinder to in-place activate a part or subassembly so you can make edits to individual assembly components while viewing the entire assembly. The PathFinder tab is available when you work in an assembly or a subassembly within the active assembly. In the Assembly environment, you can also use PathFinder to view, modify and delete the assembly relationships used to position the parts and subassemblies, reorder parts in an assembly, and to help you diagnose problems in an assembly. In the Assembly environment, PathFinder is divided into two panes. The top pane lists the components of the active assembly in a folder tree structure. Listed components can include: parts, subassemblies, assembly reference planes, and assembly sketches. The bottom pane shows the assembly relationships applied to the part or subassembly selected in the top pane. Using the top pane The top pane of PathFinder allows you to do the following: View components in collapsed or expanded form. For example, when you expand a subassembly, you can view all of its parts. Highlight, select and clear components for subsequent tasks. Determine the current status of the components within the assembly. Determine how the assembly was constructed Modeling assemblies spse01540

17 Solid Edge Assembly Reorder parts within an assembly. Rename reference planes, sketches, and coordinate systems. Place a component by dragging into the assembly from PathFinder rather than the Parts Library. When you pass your cursor over a component in the top pane of PathFinder, it is displayed in the graphics window using the Highlight color. When you click a component it is displayed using the Select color. This allows you to associate the component entry in PathFinder with the corresponding component in the graphics window. When you move the cursor over a component in the assembly window, not only does the component display in Pathfinder using the Highlight color, but if the component resides in a subassembly, any parent assemblies are also displayed in lighter shade of that color. The same rule applies after selecting a component. The component displays in PathFinder using the select color and parent assemblies show up in a lighter shade of the select color. Figure A shows PathFinder in the Highlight color and Figure B shows PathFinder in the select color, with the parent assemblies shown in a light shade of those colors. Note When you pass your cursor over or click the top-level assembly in PathFinder, it does not display in the highlight or select color. This improves performance when working with large assemblies. Because the highlight and selection of components in large assemblies can impact performance, options are available on the Assembly tab in the Solid Edge Options dialog box that allow you to improve the performance when working with large assemblies. For example, options are available that allow you to simplify the display of highlighted and selected components in the graphics window spse01540 Modeling assemblies 2-11

18 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly and to disable the highlight of components in the graphics window when you pass your cursor over them in PathFinder. For more information on improving performance in large assemblies, see the Working with large assemblies efficiently Help topic Modeling assemblies spse01540

19 Solid Edge Assembly Determining the status of a component The symbols in PathFinder reflect the current status of the components in the assembly. The following table explains the symbols used in the top pane in PathFinder: Legend Active part Inactive part Unloaded part Part that is not fully positioned Part that has conflicting relationships Linked part Assembly copy Simplified assembly Simplified part Missing component Alternate components part Part position is driven by a 2D relationship in an assembly sketch Displayed assembly Adjustable Part Adjustable Assembly Driven Reference Fastener System Pattern group Pattern item Reference planes Reference plane Sketch Noncombinable sketch (synchronous only) Combinable sketch (synchronous only) Active sketch (synchronous only) Weldment Group of parts and subassemblies Motor Available In Work In Review Released Baselined Obsolete spse01540 Limited Update or Limited Save enabled. Modeling assemblies 2-13

20 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Note The symbols in PathFinder can also represent combinations of conditions. For example, a symbol can show that a part is hidden and not fully positioned: Determining how the assembly was constructed The components in the top pane of PathFinder are listed in the order in which they were placed in the assembly. This can be useful when evaluating design changes. For example, if you delete a single assembly relationship from a part, the symbols for other parts could also change to indicate that the parts are no longer fully positioned. This occurs because the positioning of the other parts depended upon the part from which you removed the relationship. In this example, reapplying the single relationship should cause the other parts to also become fully positioned again. Making changes to assembly components You can use the top pane of PathFinder to open or in-place activate a part or subassembly so you can make design modifications. For example, you can select a part in PathFinder, then use the Edit command on the shortcut menu to in-place activate a part. You can then add, remove, or modify features on the part while viewing the other assembly components. You can also use geometry on the other assembly components to help you construct or modify features on the part. When you use the Open command to open an assembly component, you cannot view the other assembly components. When you in-place activate a subassembly, the display of PathFinder changes to make it easier to determine your current position within the assembly structure. For example, while in the top-level assembly A1.asm, if you in-place activate into subassembly S1.asm:1, subassembly S1.asm:1 is displayed using bold text and a contrasting background color is used for the subassembly and its components. When you in-place activate a part for editing, you do not need to return to the assembly first to in-place activate another part or subassembly in the assembly. You can select another part or subassembly in PathFinder and use the Edit command on the shortcut menu to in-place activate the component for editing. When you are finished making the design changes, you can use the Close and Return command on the Home tab to return to the original assembly Modeling assemblies spse01540

21 Solid Edge Assembly When you in-place activate a part or subassembly for editing, you cannot collapse the assembly structure to which the part or subassembly belongs within PathFinder. For example, in the following illustration, part P2.par:1 has been in-place activated and it is in subassembly S1.asm. If you click the minus (-) symbol adjacent to S1.asm to collapse its structure, it will remain expanded. Changing the display status of assembly components You can use the top pane of PathFinder to control the display status of assembly components. For example, you can hide parts and subassemblies to make it easier to position a new part you are placing in an assembly. You can use the checkboxes adjacent to the assembly components in PathFinder to control component display or shortcut menu commands when one or more components are selected. The color of the text in PathFinder also indicates whether a component is displayed or hidden. Reordering parts within an assembly PathFinder allows you to drag a part to a different position within an assembly. As you drag the part, PathFinder displays a symbol to show where you can reposition the part in the assembly structure. The part will be positioned below the highlighted part occurrence in PathFinder. spse01540 Modeling assemblies 2-15

22 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Grouping parts and subassemblies within an assembly PathFinder allows you to select a set of parts or subassemblies in the active assembly, then specify that the selected components are a group using the Group command on the shortcut menu. The set of components is then collected into a group entry in PathFinder. You can then expand, collapse, or rename the group to a more logical name. Defining a group of parts reduces the space requirements for a set of parts, and allows you to gather together a set of similar parts into a logical group. This can make it easier to select the parts for other operations, such as displaying and hiding a set of parts. You cannot select nested parts or nested subassemblies. Grouping components is also useful when working with large assemblies that contain few or no subassemblies. You can select a set of parts, define them as a group with the Group command on the Pathfinder shortcut menu, then use the Rename command to rename the group to a more logical name. Note Some assembly commands create a group of components automatically. For example, the Move Components command creates a group entry in PathFinder when you set the Copy option on the command bar. You can ungroup a group using the Ungroup command on the shortcut menu when a group is selected in PathFinder. The Select Components command, on the shortcut menu when you select a group entry in PathFinder, activates additional commands and options for manipulating groups that would otherwise be disabled. For example, after selecting a group with the Select Components command, you can then apply a face style to the group of parts, or transfer the group of parts to another assembly. Renaming PathFinder entries You can use PathFinder to rename an entry for an assembly reference plane, sketch, group, or coordinate system. To rename an entry, select it in PathFinder, right-click and then click Rename. In the name box, type the new name for the entry Modeling assemblies spse01540

23 Solid Edge Assembly Finding parts In a complex or unfamiliar assembly, it can sometimes be difficult to determine which subassembly a particular part is contained in. You can use the Scroll To command to quickly find a part in PathFinder. When you select a part in the assembly window, then click the Scroll To command on the shortcut menu, the display of PathFinder scrolls to the selected part. If the part is in a subassembly, the listing for the subassembly is expanded to display the part. To automatically scroll to a selected part, set the option Auto scroll in assembly pathfinder, on the assembly tab in Solid Edge options. When this option is set, pathfinder scrolls so that the selected part is visible in pathfinder. This is useful when working in large assemblies. Replacing the file name with the document name formula value You can use the Document Name Formula dialog box to replace the file name displayed in PathFinder with a value composed of document properties. Refer to the Replace a file name with a property value help topic for instructions. You can combine properties with additional characters to replace the file name. For example, you can separate two properties with dashes, such as Document Number Revision Number. If a property does not exist or does not have a value, the property name is displayed in place of the property value, and the file name is displayed in parentheses after the value. Note The Property list displays the properties that you can use to replace the file name. You can add a property that is not in the active document by typing [property name] in the Formula field. spse01540 Modeling assemblies 2-17

24 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Using the bottom pane When you select a part or subassembly in the top pane of PathFinder, you can use the bottom pane to view and modify the assembly relationships between the selected part and the other parts in the assembly. The document name is also displayed, as well as a symbol that represents the type of relationship. The following table explains the symbols used in the bottom pane in PathFinder: Legend Ground relationship Mate relationship Planar align relationship Axial align relationship Connect relationship Angle relationship Tangent relationship Cam relationship Rigid set relationship Center plane relationship Gear relationship Suppressed relationship Failed relationship Driving relationship, such as a linked assembly driven part feature. When you select a relationship in the bottom pane you can do the following: View which elements were used to apply the relationship. Edit the fixed offset value of the relationship. Change the offset type of the relationship. Delete the relationship. Suppress the relationship Note Double-click a relationship to display the edit dialog box for that relationship. When editing a relationship with missing geometry double click or edit definition will take you into a step to select and fix the missing geometry. Shortcut menu for relationships The shortcut menu for a relationship in the lower pane of PathFinder has the following commands: 2-18 Modeling assemblies spse01540

25 Solid Edge Assembly Show Show only Zoom to Note Zoom to is useful for finding the geometry used to define a relationship in large assemblies. Select Components Note Select components puts the two components used to define the relationship into a selection set. Viewing assembly relationships When you select a relationship in the bottom pane, the elements used to apply the relationship are highlighted in the assembly window. For example, if you select a planar align relationship, the planar faces or reference planes that were used to apply the relationship highlight in the assembly window. This can help you determine how design changes need to be applied. Modifying assembly relationships When you select a relationship in the bottom pane, you can use the relationship command bar to edit the fixed offset value or change the offset type. For example, you may want to change a mate relationship from a fixed offset to a floating offset. Note If you change the offset type from fixed to floating, you may have to make other relationship edits to ensure that the part remains fully positioned. Deleting assembly relationships If you delete an assembly relationship, the symbol next to the part in the top pane changes to show that the part is no longer fully positioned. The part is also placed on the Error Assistant dialog box list. It is good practice to apply a new relationship to the affected parts as soon as possible. If you delete too many relationships without applying new ones, it could become difficult to fully position the affected parts. If this occurs, you may have to delete the affected parts from the assembly and place them again. spse01540 Modeling assemblies 2-19

26 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Replacing relationships After you place a part in an assembly, you can replace any of its relationships. Select the part in PathFinder or in the graphics window, then click the Edit Definition button on the command bar. You can then select the relationship you want to replace from the Relationship List box on the command bar. Use the Relationship Types button to specify the new relationship you want to apply. Note You can also delete the current relationship in the bottom pane of PathFinder and apply a new one using the Assemble command bar. Conflicting relationships If you change the design of parts in an assembly, some assembly relationships may no longer be applicable. When this occurs, the symbol next to the part or subassembly in the top pane of PathFinder will change to indicate that there are conflicting relationships and the part will be placed on the Error Assistant dialog box list. When you select the conflicted part or subassembly, the symbols for the affected relationships in the bottom pane of PathFinder are displayed in red. You can then evaluate the relationship scheme to determine how to repair the assembly. For example, you can delete the affected relationships and apply new relationships to fully position the part. Suppressing assembly relationships You can use the Suppress command on the shortcut menu to temporarily suppress an assembly relationship for a part. Suppressing an assembly relationship allows you to use the Drag Part command to evaluate how the part interacts with other parts in the assembly. When you suppress an assembly relationship, the symbol for the part in the top pane of PathFinder changes to indicate that the part is no longer fully positioned. Also, a symbol is added adjacent to the suppressed relationship in the bottom pane to indicate that the relationship is suppressed. Note You can use the Unsuppress command on the shortcut menu to unsuppress the relationship. Displaying document status in PathFinder You can display the document status for components in PathFinder. For example, in an Insight-managed document, the status can be Available, In Work, In Review, Released, Baseline or Obsolete. The Status Display Status command on the PathFinder shortcut menu turns on and off the display of symbols adjacent to the document names in PathFinder Modeling assemblies spse01540

27 Solid Edge Assembly Legend Available In Work In Review Released Baselined Obsolete Dashed line in the bottom pane Often a dashed line is displayed between sets of relationships in the bottom pane of PathFinder. The relationships above the dashed line were applied to parts that are above the selected part in the top pane of PathFinder. The relationships below the dashed line were applied to parts that are below the selected part in the top pane of PathFinder. You can edit the relationships above the dashed line and below the dashed line. For example, when you select Valve01.asm, the relationships above the dashed line were applied to Body01.par, which is above Valve01.asm in the top pane of PathFinder. The relationships below the dashed line were applied to Handle01.par and NutM15.par, which are below Valve01.asm in the top pane of PathFinder. Managing relationships in nested assemblies PathFinder can show relationships applied outside the active assembly. You can view the relationship by clicking the part in PathFinder. spse01540 Modeling assemblies 2-21

28 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Understanding Assembly relationships Developing an understanding of the various assembly relationships is fundamental to successfully creating assemblies. When you place a part or subassembly into an assembly, you define how the part is positioned with respect to the other parts by applying assembly relationships. Available relationships include Mate, Planar Align, Axial Align, Insert, Connect, Angle, Tangent, Cam, Path, Parallel, Gear, Match Coordinate System, Center-Plane, Rigid Set, and Ground (see Show list of assembly relationships for additional information). In addition to the traditional assembly relationships listed above, the FlashFit option reduces the steps required to position a part using the Mate, Planar Align, or Axial Align relationships. All relationship options in addition to the FlashFit option are located on the Assemble - Relationship Types list on the Assemble command bar and the relationship-specific command bars for each type of relationship. Part positioning workflows The following workflows are used to position parts in an assembly: FlashFit workflow Traditional workflow Reduced Steps workflow Capture Fit workflow Note If you are new to modeling, focus on learning both FlashFit and the Traditional workflows. As your expertise in building assemblies increases, explore the other available workflows. All workflows are discussed in more detail later in this topic. The Slider tutorial demonstrates FlashFit capabilities Modeling assemblies spse01540

29 Solid Edge Assembly Maintaining assembly relationships By default, Solid Edge maintains the relationships that are defined when the part is position. If the Maintain Relationships option is set on the Parts Library shortcut menu (right-click on the white space in the Parts Library) when a part is placed, the relationships that are applied also control the behavior of the part when it is modified. For example: If a Planar Align relationship is applied between two parts, they remain aligned when either part is modified. If an Axial Align relationship is applied between two parts, they remain axially aligned when either part is modified. Note Assembly relationships can be viewed, modified, or deleted using the Assembly PathFinder. If the Maintain Relationships command is cleared when a part is placed, the assembly relationships must still be used to position the part in the assembly. However, instead of applying these relationships on the part, the software applies a Ground relationship. Grounded parts do not update their positions in the assembly when other parts are modified. spse01540 Modeling assemblies 2-23

30 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Capturing design intent To fully control one part in relation to the other parts in an assembly, a combination of assembly relationships must be applied. There is often more than one way to apply relationships that will position a part correctly. It is important to choose the way that best captures design intent, because this makes the assembly easier to understand and edit. It may be helpful to keep in mind how the part will react to future modifications when positioning a part. Although the part may be positioned correctly using a particular set of assembly relationships, it may not behave as expected if modifications are made. To gain more experience placing parts in an assembly, it can be useful to make minor design modifications and observe how the parts in the assembly react. If the assembly does not behave as expected, relationships can be deleted and reapplied using a different approach. With more experienced, it will become easier to see which set of relationships correctly position parts and also provide the desired design intent behavior when design modifications are made later in the process. Assembly relationships and part movement When a part is fully positioned in an assembly, it cannot move in any direction in relation to the assembly. The first assembly relationship that is placed controls some part movement, but the part is still free to move in some other direction by sliding along or rotating around the X, Y, or Z axes. Applying more relationships controls more movement until the part is fully positioned. The types of relationships and options that are applied determine how the relationships control part movement. Of course parts that must be able to move in an assembly cannot be fully positioned. This is generally achieved by defining rotational relationships that are not locked, ranges of motion that allow movement, or floating relationships that determine the extent of movement as defined by another part or subassembly. Parts can also be made to be adjustable (see Adjustable and rigid assemblies for more information) Modeling assemblies spse01540

31 Solid Edge Assembly FlashFit workflow The FlashFit workflow reduces the steps required to position parts using Mate, Planar Align, and Axial Align relationships when compared to the traditional workflow. Because many parts are positioned using these relationships, FlashFit is appropriate and quicker in many situations. The FlashFit relationship is the default assembly relationship which makes the FlashFit workflow the default workflow. This default condition is controlled through the Assemble Command bar Options dialog box. When possible, FlashFit moves the first part that was selected when applying the relationship while the second part remains stationary. If the first part is fully constrained, the second part will move. The FlashFit option can then be used to define additional relationships required to fully position the part in the assembly, or select another relationship type can be selected. Note When placing a subassembly using the FlashFit or Reduced Steps workflows, the parts in the subassembly must be active before anything can be selected. If the subassembly is not already active, it can be activated using the Activate Part button on the Assemble command bar. If a face, edge, or point on the placement part cannot be selected the most common reason is that the part in the subassembly has not been activated. Using FlashFit for positioning fasteners FlashFit also allows more flexibility to use edges, in addition to faces, when positioning a part using mate, axial align, and planar align relationships. This can be especially useful when positioning a fastener, such as a bolt into hole. For example, when positioning a part using an Axial Align relationship, a circular edge cannot be selected. However when using FlashFit, a circular edge on both the placement part and target part can be selected to completely position the part in two steps. FlashFit options The Options dialog box on the Assemble command bar is used to set which FlashFit options to consider when placing a part. For example, any combination of the following element types can be specified to placing a part; Planer faces, Cylindrical faces, Linear edges, or Points. This allows the behavior of the FlashFit command to be tailored for the part that is currently being placed. This action can help limit the number of identified elements to only those specific elements being sought when applying a relationship. Moving and rotating parts with FlashFit When using FlashFit, the placement can be moved or rotated into a more convenient location. To move the part, position the cursor over the part and drag the cursor. To rotate the part, press the Ctrl key while dragging the cursor. If any relationships have already been applied to the placement part, the movement or rotation is limited to the available degrees of freedom. spse01540 Modeling assemblies 2-25

32 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Traditional workflow The traditional workflow requires the user to perform each step required to position a part using assembly relationships. This approach allows new users to gain a full understanding of the part positioning process. The Assembly command bar and displayed prompts, that are unique to each type of relationship, guide the user through the positioning process. The traditional workflow is also preferred when positioning parts using relationships that FlashFit does not recognize, such as Angle, Cam, Parallel, Path, and Tangent relationships. Reduced Steps workflow The Reduced Steps workflow eliminates the part selection and accept steps in the traditional workflow. To use this option activate the Use Reduced Steps when placing parts in the Options dialog box on the Assemble command bar (see Assemble Command bar Options dialog box for more information). When the Use Reduced Steps when placing parts option is set, simply select a face on the placement part and target part to form a relationship. This reduces the number of steps from five to three for a typical Mate relationship. There are some trade-offs when using this option. Since the part in the assembly is no longer selected as a separate step, surfaces or cylinders on every active part are available for selection. In large assemblies or in assemblies with numerous overlapping parts, positioning one part precisely to another can prove time consuming. In such cases, use the QuickPick option to select the relationship feature. Note When the Use Reduced Steps when placing parts option is set, the offset type and offset value must be set before selecting the target face. To use a reference plane on the target part to position the placement part, the reference planes must already be displayed. Capture Fit workflow The Capture Fit workflow uses the Capture Fit command to save assembly relationships and faces used to position a part or subassembly in the active assembly. When the part or subassembly is placed again, simply select the faces on a new target part already in the assembly to position the new part or subassembly. This reduces the number of steps required to position the part. If the Insert option is used to position a part, the Capture Fit command will capture a mate and an axial align relationship, since these are the relationships that the Insert option actually places. Relationships can also be captured by activating the Automatically Capture Fit when placing parts option on the Options dialog box on the Assemble command bar. Note The Capture Fit command cannot capture angular relationships Modeling assemblies spse01540

33 Solid Edge Assembly Defining offset values Fixed or floating offsets between the parts can de defined for some types of relationships such as Mate and Planer Align. To specify an offset type, select one of the offset type options on the Assemble command bar; Fixed, Float, or Range. When a fixed offset is selected, enter the dimensional value for the offset distance. For example, when a fixed offset for a planar align relationship is defined, a value can be set so that the parts are no longer coplanar. A floating offset is useful when the orientation of a part with respect to another part needs to be controlled but it is impossible to define a fixed dimensional value. For example, a floating offset can be applied to control the rotational orientation of a part. When an Axial Align relationship is applied using the Unlock Rotation option between a cylindrical shaft and the cylindrical axis on another part as shown in (A), then a Planar Align relationship using a Float option can control the rotational orientation of the shaft as shown in (B). Attempting to apply a fixed offset using a Planar Align relationship results in displaying a message that indicates that the relationship conflicts with another relationship. Note The range offset command is not intended to be used to for geometric tolerances. Depending on the relationships used to position the part are defined, this may result in an over constrained condition and cause errors. spse01540 Modeling assemblies 2-27

34 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Locking and unlocking rotation on axial align relationships When an Axial Align relationship has been applied, use the Lock Rotation and Unlock Rotation buttons on the Assemble command bar to specify whether the part is free to rotate around the axis of rotation. The Lock Rotation option is useful when the rotational orientation of the part is not important, such as placing a bolt into a hole. When the Lock Rotation option is selected, the rotational orientation of the part is locked at a random position and one less relationship is required to fully position the part. When the Unlock Rotation option is set, the rotational orientation can be set to the desired condition by applying another relationship such as an Angle relationship. Assembly relationship dimensions When positioning parts using assembly relationships, driving or driven dimensions are created and displayed when appropriate. For example, when a part is positioned using a Mate relationship with a fixed offset, a driving dimension is created. When a part is positioned using a Mate relationship with a floating offset (the offset value is controlled by another relationship), a driven dimension is created that cannot be edited to reposition the part. Zero, positive, and negative dimension values are supported. When an assembly relationship is first applied or later edited, the driving dimension can be selected to change the offset value Modeling assemblies spse01540

35 Solid Edge Assembly Assembly Relationship Assistant command When working with assemblies whose parts are oriented correctly, but do not have assembly relationships, such as assemblies that were imported into Solid Edge from another CAD system, the Assembly Relationship Assistant command can be used to apply relationships between the parts and subassemblies. The relationships are applied based on their current geometric orientation. For more information, see the Assembly Relationship Assistant command Help topic. Differences between assembly relationships and sketch relationships The relationships that are applied between the parts and subassemblies of an assembly differ from the relationships that are applied while working with part sketches. For example: There are no relationship handles added to the assembly to show that a relationship has been applied. Instead, the relationships between parts are shown in the PathFinder. Except for the ground relationship, all assembly relationships are defined between the part or subassembly that is being placed and a part or subassembly that was previously placed in the assembly. The dimensioning commands cannot be used to place relationships between parts and subassemblies in an assembly. Positioning parts using coordinate systems Parts can also be placed in an assembly using coordinate systems. To accomplish this, the coordinate systems in the part document for both the placement and target parts must be defined. Then use the Planar Align, Mate, and Match Coordinate Systems options on the Assemble command bar to position the placement part. For example, when using the Match Coordinate Systems option, the placement part is positioned using planar align relationships that match the three principal axes on the coordinate system for the placement part and the target part. This allows the placement part to be positioned using fewer steps than applying three separate planar align relationships. This can be useful when working with a common part that is placed into an assembly multiple times in the same position relative to a target part. spse01540 Modeling assemblies 2-29

36 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Capture Fit command Use the Capture Fit command to capture the assembly relationships and faces used to position a part or subassembly already placed in the assembly. You can then place the part or subassembly again later using fewer steps. You can use the Capture Fit dialog box to specify which relationships you want to capture. If you used the Insert option to position a part, the Capture Fit command will capture a mate and an axial align relationship, since these are the relationships that the Insert option actually places. You can also capture relationships by setting the Automatically Capture Fit When Placing Parts option on the Options dialog box on the Place Part command bar. Note The Capture Fit command cannot capture angular relationships Modeling assemblies spse01540

37 Solid Edge Assembly Capture the assembly relationships for a part 1. In the assembly window, select a part for which you want to capture relationships. 2. Choose Home tab Relate group Capture Fit. 3. In the Capture Fit dialog box, use the Add and Remove buttons to specify which relationships you want to capture, and then click OK. Tip You can also select the part you want to use in PathFinder. When you use the Capture Fit command, the relationships and faces used to position the part or subassembly the first time are stored so you can place the part using fewer steps later. If you used the Insert option to position a part, the Capture Fit command will capture a mate and an axial align relationship, since these are the relationships that the Insert option actually places. The Capture Fit command cannot capture angular, cam or center-plane relationships. You can also capture relationships by setting the Automatically Capture Fit When Placing Parts option on the Options dialog box on the Place Part command bar. spse01540 Modeling assemblies 2-31

38 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Activity: Positioning parts with Mate, Axial Align, Planar Align and Insert Overview This activity shows the process of positioning parts using Mate, Axial Align, Planar Align and Insert. The parts will be positioned with the Reduced Steps option turned off to better understand the workflow options in the command bar. Then the same parts will be placed with the Reduced Steps option turned on to show how the process can be streamlined. Note FlashFit is a preferred method of quickly positioning parts in an assembly and will be covered in another activity. This activity forces you to manually position parts so that you will understand what is occurring when parts are positioned using Flashfit and how to change a single relationship to reposition a part if an edit is later required. Objectives Parts will be added to an assembly using the commands Mate, Planar Align, Axial Align and Insert In this activity you will: Learn how to position parts using the commands Mate, Axial Align, Planar Align and Insert without using Reduced Steps. Learn how the command bar reflects the workflow during the positioning of parts. Use reduced steps to position parts with Mate, Planar Align, Axial Align, and Insert. Activity In this activity you will learn the procedure for positioning parts in an assembly using the Mate, Planar Align and Axial Align relationships Modeling assemblies spse01540

39 Solid Edge Assembly Overview This activity will position a part with reduced steps turned off to show the complete sequence of steps involved in positioning a part. The second part will be placed with reduced steps turned on to show a more efficient method of positioning parts. spse01540 Modeling assemblies 2-33

40 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Create a new assembly and position the first part In this step, you will create a new assembly using the ISO Metric Assembly template. The Insert Component command will display the Parts Library. In the Parts Library, you will browse to the folder containing the training files and place them into the assembly by drag and drop. Create a new assembly file using the ISO Metric Assembly template. After the assembly document opens, click the Application button. Choose Solid Edge Options, and then click the Assembly tab. Check the box as shown. On the Home tab in the Assemble group, click the Insert component command to display the parts library. Browse to the folder containing the training files for this activity. From the Parts Library in PathFinder, drag the part dome.par in the assembly window. Note The first part placed in the assembly is placed as a grounded part Modeling assemblies spse01540

41 Solid Edge Assembly Applying a Mate relationship In this step you will apply a Mate relationship between two parts. Tip If you select the wrong face in a step, you can back up by clicking the button corresponding to that step on the command bar, and then selecting the proper geometry again. Drag the part a1_part.par into the assembly window. Click the Options button on the command bar. Set the options shown and then click OK. Make sure the reduced steps option is off and FlashFit as the default placement method is off. Select the Mate relationship. Note The command bar reflects the current placement step in the workflow. Notice the current step is the Placement Part - Element step, and you are being prompted to select an element on the placement part. spse01540 Modeling assemblies 2-35

42 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly For this relationship, select the face shown. Note The command bar shows the Target Part step is active, and you are being prompted to select the target part. This part has the face you will apply the Mate relationship to Modeling assemblies spse01540

43 Solid Edge Assembly Select the target part, dome.par as shown. Note Notice the Target Part - Element step is active, and you are being prompted to select the target part element. This element is the face the Mate relationship will be applied to. spse01540 Modeling assemblies 2-37

44 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the face shown on dome.par. Right-click or click the OK button to Accept. The Mate relationship is applied Modeling assemblies spse01540

45 Solid Edge Assembly Applying a Planar Align relationship The relationship list on the command bar increments after each relationship is applied. Relationship 2 will be a Planar Align relationship between faces in both parts. Set the relationship type to Planar Align. Select the face shown. spse01540 Modeling assemblies 2-39

46 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the target part shown. This part has the face you will apply the Planar Align relationship to Modeling assemblies spse01540

47 Solid Edge Assembly Select the face shown. This is the face you will apply the Planar Align relationship to. Right-click or click the OK button to accept. The Planar Align relationship is applied. spse01540 Modeling assemblies 2-41

48 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Applying an Axial Align relationship The relationship list increments to the next relationship. Relationship 3 will be an Axial Align. Set the relationship type to Axial Align. Note The Locate Steps group on the command bar reflects the current placement step in the workflow. For this relationship, you will select a cylindrical axis. Select the cylindrical axis shown Modeling assemblies spse01540

49 Solid Edge Assembly Note The Locate Steps group on the command bar reflects the current placement step in the workflow. This part has the cylindrical axis you will apply the Axial Align relationship to. Select the target part shown. Note The Locate Steps group on the command bar reflects the current placement step in the workflow. This element is the cylindrical axis you will apply the Axial Align relationship to. spse01540 Modeling assemblies 2-43

50 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the cylindrical axis shown. Right-click or click OK to accept. The Axial Align relationship is applied, and the part is fully positioned Modeling assemblies spse01540

51 Solid Edge Assembly Applying a Mate relationship with Reduced steps Another occurrence of the part a1_part.par will be placed. The sequence of steps will be the same except Reduced Steps will be used. Note When the Reduced Steps option is used, the step for selecting the target part is eliminated. Valid features on every part are available for selection and the target part is determined from the part containing the feature. This option is more efficient in most cases, however in large assemblies where an area can be congested with many parts, it is desirable to have more control by manually choosing the target part as was shown in the previous steps. From the Parts Library, drag the part a1_part.par into the assembly window. You will apply a Mate relationship. Click the Options button on the command bar. Set the options shown. Make sure the Reduced Steps option is on and FlashFit as the default placement method is off. Select the Mate relationship. Note The command bar reflects the placement step in the workflow. Notice the step is currently the element step and you are being prompted to select an element of the placement part. For this relationship, you will select a face. spse01540 Modeling assemblies 2-45

52 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the face shown. Note Because the Reduced Steps option is set, the command bar reflects the placement step in the workflow. Notice the step is now the target part element, and you are being prompted to select the target part element. This element is the face the Mate relationship will be applied to. The target part is automatically assigned and is the part on which the target element belongs Modeling assemblies spse01540

53 Solid Edge Assembly Select the face shown. The Mate relationship is applied. Note Using Reduced steps, there is no need to click OK to complete. Once the target element is selected, the relationship is established. spse01540 Modeling assemblies 2-47

54 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Applying a Planar Align relationship with reduced steps Once this relationship is established, the relationship list increments to the next relationship. Relationship 2 will be a Planar Align. Set the relationship type to Planar Align. Note The command bar reflects the placement step in the workflow. Notice the step is currently the element step and you are being prompted to select an element of the placement part. For this relationship, you will select a face. Select the face shown Modeling assemblies spse01540

55 Solid Edge Assembly Note The command bar reflects the placement step in the workflow. Notice the step is now the target part element, and you are being prompted to select the target part element. This element is the face you will apply the Planar Align relationship to. Select the target part element shown. The Planar Align relationship is applied. spse01540 Modeling assemblies 2-49

56 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Applying a Axial Align relationship with Reduced Steps Once this relationship is established, the relationship list increments to the next relationship. Relationship 3 will be an Axial Align. Set the relationship type to Axial Align Note The command bar reflects the placement step in the workflow. Notice the step is currently the element step and you are being prompted to select an element of the placement part. For this relationship, you will select a cylindrical axis. Select the cylindrical axis shown Modeling assemblies spse01540

57 Solid Edge Assembly Note The command bar reflects the placement step in the workflow. Notice the step is now the target part element, and you are being prompted to select the target part element. This element is the cylindrical axis you will apply the Axial Align relationship to. spse01540 Modeling assemblies 2-51

58 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the cylindrical axis shown. The Axial Align relationship is applied, and the part is fully positioned Modeling assemblies spse01540

59 Solid Edge Assembly Placing a fastener with the Insert command Insert will be used to position a fastener in a hole. Note Insert requires a Mate and an Axial Align. Once you have established these relationships, the rotation of the aligned axis is locked and the part is fully positioned. Drag the part 10mm_fastener.par into the assembly window. Select the Insert Command. Note The Mate relationship will be established first, then the Axial Align. Because of the number of faces to choose from, Quickpick will be used to aid in the selection. Fort the Mate relationship, select the face shown. spse01540 Modeling assemblies 2-53

60 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the target face for the Mate relationship as shown. For the Axial Align relationship, select the cylindrical axis shown Modeling assemblies spse01540

61 Solid Edge Assembly For the target face of the Axial Align relationship, select the face shown. The fastener is placed and fully positioned, with the rotation locked. Click the Select Tool to exit. Close the assembly document without saving. Note An equivalent and more efficient way of placing fasteners is done by matching circular edges of the fastener and the hole using FlashFit. This is covered in another activity. spse01540 Modeling assemblies 2-55

62 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Summary In this activity you learned the workflow for establishing relationships needed to position parts in an assembly. You also learned that using the reduced steps option streamlines the process of positioning parts Modeling assemblies spse01540

63 Solid Edge Assembly Activity: Placing parts in an assembly using FlashFit Overview In this activity, FlashFit will be used to position parts in a valve assembly. Objectives The objective of this activity is for you to be able to use appropriate relationships to position parts in an assembly. Activity In this activity you will learn the procedure for positioning parts in an assembly using FlashFit to achieve the relationships of Mate, Planar Align and Axial Align. spse01540 Modeling assemblies 2-57

64 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Overview You will use FlashFit to position parts and subassemblies in completing the valve assembly Modeling assemblies spse01540

65 Solid Edge Assembly Place the first part in the assembly. Create a new assembly and place the first part. Create a new ISO metric assembly file. Click the Insert Component, click the Parts Library and drag st_v_housing.par into the assembly window. The first part placed in a new assembly file is grounded. spse01540 Modeling assemblies 2-59

66 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Use FlashFit to position the valve parts and subassemblies Use FlashFit to position the valve parts. Before placing additional parts, set the FlashFit parameters. Once the parameters are set, the part will be positioned. From the Parts Library, drag the subassembly st_v_handleball.asm into the assembly window. Click the Options button on the command bar. Set the Options shown and then click OK. Set the relationship type to FlashFit Modeling assemblies spse01540

67 Solid Edge Assembly Select the circular edge shown. Use QuickPick for an accurate selection. Note Matching circular edges with FlashFit is the equivalent of using the Insert command. A Mate relationship, and an Axial Align relationship with locked rotation is created. spse01540 Modeling assemblies 2-61

68 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the inner lip of the center hole of the housing. The subassembly is positioned Modeling assemblies spse01540

69 Solid Edge Assembly Place the remaining parts Place additional parts in the assembly until finished. Drag st_v_endplate.par into the assembly window. Use QuickPick to select the face shown. spse01540 Modeling assemblies 2-63

70 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Select the target face on the housing as shown. A Mate relationship is applied. The next two relationships will be established using alignment of holes in the parts. Select the cylindrical axis on the st_v_endplate.par as shown Modeling assemblies spse01540

71 Solid Edge Assembly For the target, select the cylindrical axis shown. An Axial Align relationship is applied. For the last relationship needed to completely position the part, select the cylindrical axis shown. spse01540 Modeling assemblies 2-65

72 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly For the target, select the cylindrical axis shown. An Axial Align relationship is applied and the part is positioned. Drag another occurrence of st_v_endplate.par into the assembly window Modeling assemblies spse01540

73 Solid Edge Assembly Place st_v_endplate.par on the opposite side of the housing from the one just place using the same procedure you used to place the previous part. Note FlashFit will assign either a Mate or a Planar Align to flat faces based on the closest orientation of the two faces being positioned. In this case, if a Planar Align is assigned rather than a Mate, use the flip button to change the relationship type to a Mate. Drag st_v_top.par into the assembly window. spse01540 Modeling assemblies 2-67

74 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Use FlashFit to position st_v_top.par as shown. The procedure is similar to the one used to place the previous two parts. Drag 10mm_fastener.par into the assembly window. Using QuickPick, select the circular edge shown Modeling assemblies spse01540

75 Solid Edge Assembly For the target, select the circular edge shown on the top cap. The fastener is placed. Place additional occurrences of 10mm_fastener.par in the remaining holes on the valve using the same procedure. Note spse01540 Modeling assemblies 2-69

76 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly If FlashFit positions the fasteners incorrectly as shown, follow the steps outlined to correct the placement. The reason for the incorrect placement of the fastener is that FlashFit determines whether to apply a Planar Align or a Mate relationship to the fastener based on the orientation of the face relative to the placement face. If the part faces are closer to a Planar Align relationship, then that is what is applied. Prior to selecting the circular edges in FlashFit, the fastener can be rotated into the approximate desired orientation by holding CTRL while dragging it. This will result in correct placement and is easier than correcting the placement using Flip outlined below. Click the Select command. Select the fastener. In the lower pane of PathFinder, right-click the Planar Align relationship, and then click Flip Modeling assemblies spse01540

77 Solid Edge Assembly This completes the activity. Close the assembly document without saving. spse01540 Modeling assemblies 2-71

78 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Summary In this activity you learned how to place parts and subassemblies from a Parts Library and position them in an assembly. FlashFit consists of the Mate, Planar Align and Axial Align relationships and determines which is appropriate. When using FlashFit and selecting circular edges, fasteners can quickly be positioned because the rotation of the fastener is locked and the part becomes fully constrained Modeling assemblies spse01540

79 Solid Edge Assembly Lesson review Answer the following questions: 1. What are the steps required to apply a mate relationship without using flashfit or reduced steps? 2. What is the difference between mate and planar align? 3. What is a floating offset? 4. Are linear edges valid for the placement of an axial align relationship? 5. When using reduced steps, which step is eliminating when creating a relationship? spse01540 Modeling assemblies 2-73

80 Lesson Lesson 2: 2: Solid Solid Edge Edge Assembly Assembly Lesson summary In this lesson you learned the workflow for establishing relationships needed to position parts in an assembly. You also learned that using the reduced steps option streamlines the process of positioning parts Modeling assemblies spse01540

81 Lesson 3: More Assembly Relationships Relationships position the selected part or subassembly into the active assembly. Parts are positioned in assemblies using a combination of assembly relationships. Relationship List Lists the relationships applied to the part. You can replace a previously applied relationship by selecting a relationship from the list and then selecting a new relationship from the Relationship Types list. Relationship Types Lists the assembly relationship types you can apply. Parts can be positioned using the following relationship options: Mate Planar Align Apply a mate relationship between parts Modify the fixed offset value for a mate relationship Mate command Mate command bar Apply a Planar Align Relationship Between Parts Planar Align command Planar Align command bar Axial Align Apply an axial align relationship Insert Connect Ground Angle Axial Align command Axial Align command bar Insert a part in an assembly Insert command (Assembly Environment) Insert command bar Apply a Connect Relationship Between Parts Connect command (Assembly environment) Connect command barr Apply a ground relationship to a part in an assembly Ground command Apply an Angle relationship between parts Angle command Angle command bar spse01540 Modeling assemblies 3-1

82 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Tangent Cam Parallel Apply a Tangent relationship between parts Tangent command (Assembly environment) Tangent command bar (Assembly Environment) Apply a cam relationship Cam command Cam command bar Apply a parallel relationship between two parts in an assembly Parallel command (Assembly environment) Parallel command bar Center-PlaneApply a Center-plane relationship Match Coordinate Systems Center-plane command Center-Plane command bar Position two parts by matching their coordinate systems Match Coordinate Systems command Match Coordinate Systems command bar Gear/MotionPlace a gear relationship Path Rigid Gear command Gear command bar Apply a path relationship Path command Path command bar Place a Rigid Set relationship Rigid Set command Rigid Set command bar Note The Insert option applies a mate relationship with a fixed offset value and an axial align relationship with its rotational value fixed. 3-2 Modeling assemblies spse01540

83 More Assembly Relationships Connect Relationship Applying a connect relationship When two parts in an assembly cannot be positioned properly by mate and align relationships, you can position them using connect relationships. A connect relationship positions a keypoint on one part with a keypoint, line, or face on another part. For example, you can apply a connect relationship to position the center of a spherical face on one part with respect to a spherical face on another part. You can use the following methods to apply connect relationships: Point-to-Point: In the following figure, a mate relationship is applied between the mitered corners of the parts. A connect relationship, which ties a point on one part to the appropriate point on another, connects the two corners properly. A floating align relationship between the back surfaces fully positions the part. spse01540 Modeling assemblies 3-3

84 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Point-to-Line: In the following example, a mate relationship is applied between the faces of the two parts. Because the sides of each part are drafted, there are no part faces which you can use to apply a planar align relationship. You can apply three connect relationships between the keypoints on the top part and the linear edges on the bottom part. Point-to-Plane: In the following example, the lower right pin is positioned to a depth that just touches the surface of a reference plane. 3-4 Modeling assemblies spse01540

85 More Assembly Relationships Cone-to-Cone: In the following example, the cone on the fastener is connected to the cone on the countersunk hole on the plate. When you add a connect relationship between two conical faces, the keypoint that represents the theoretical intersection of the individual cones are connected. You can also apply an offset value to a connect relationship between two conical faces. spse01540 Modeling assemblies 3-5

86 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Activity: Positioning assembly parts using the Connect relationship Overview The objective of this activity is to position a part in an assembly using the Connect relationship. Activity In this activity you will use the Connect relationship to position a part. The faces of the parts have draft angles and because of this the Connect relationship will need to be used rather than the Planar Align relationship. 3-6 Modeling assemblies spse01540

87 More Assembly Relationships Overview This activity shows several options available that are used to position parts within an assembly using the Connect relationship. Objectives You will open an assembly with several unconstrained parts. You will use the Connect relationship to position the parts. spse01540 Modeling assemblies 3-7

88 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Open the assembly Open Connect.asm and activate all the parts. Click the Application button. Click Settings Options for Solid Edge Options, and then click the Assembly tab. Check the box as shown. 3-8 Modeling assemblies spse01540

89 More Assembly Relationships Position the lid by connecting 3 points Use the Connect relationship to position the lid. Position the lid by connecting three of the corner arc centers together. This will completely position the lid. Note The Connect relationship recognizes key topological features to position parts. Like the Axial Align option, linear edges can be connected. Endpoints and midpoints of linear elements are valid for connecting, as well as arc and circle centers. Set the display to Visible and Hidden Edges. By exposing the hidden edges, it is easier to locate the desired connection geometry. Click the Select command, and then select the lid shown. To position the part, click the Edit Definition button. Set the relationship type to Connect. spse01540 Modeling assemblies 3-9

90 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Select the point on the arc center of the lid as shown. Select the corner of the other lid shown as the target point for the first relationship Modeling assemblies spse01540

91 More Assembly Relationships Repeat these steps for any two of the remaining three corners. The lid is then completely positioned. spse01540 Modeling assemblies 3-11

92 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Use spherical faces to define a connect relationship Position the center of the sphere on the knob to the center of the half sphere depression in the lid. This shows how spherical faces can be positioned using the Connect relationship. Click the Select Tool and select the knob. Then click the Edit Definition command as shown. Set the relationship type to Connect. Select the face of the sphere on the knob as shown. As the target, select the face shown. You may need to use QuickPick to make the selection more efficient Modeling assemblies spse01540

93 More Assembly Relationships Note The center of the sphere on the knob is now connected to the center of the spherical depression on the face. The knob has freedom to pivot about this point. Other relationships, such as Mate with a floating offset can be used to exactly position the knob. As an optional step in this activity, use the Mate relationship to completely position the knob as shown. You may also want to use the parts reference planes to help position the knob. Close the assembly without saving. This completes the activity. spse01540 Modeling assemblies 3-13

94 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Summary In this activity you learned to use the Connect relationship to position a lid using points, and to position a knob by connecting sphere centers together. This activity is complete Modeling assemblies spse01540

95 More Assembly Relationships Activity: Positioning assembly parts using the Angle relationship Overview The objective of this activity is to position a part using the Angle relationship. Activity In this activity you will position a part using the Angle relationship, then modify the value of the angle and observe the change in position. spse01540 Modeling assemblies 3-15

96 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Overview This activity shows several options that are used to position parts within an assembly using the Angle relationship. Objectives You will open an assembly with unconstrained parts, and then use the Angle relationship to position the parts Modeling assemblies spse01540

97 More Assembly Relationships Open the assembly Open Angle.asm with all the parts active. spse01540 Modeling assemblies 3-17

98 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Create a Connect relationship To position the lid, the first relationship you establish will be the Connect relationship. Click the Select command and select the part shown. Then click the Edit Definition button as shown. Select the Connect relationship Modeling assemblies spse01540

99 More Assembly Relationships Choose Assemble Options, and turn on the points option for Flashfit. Check the box as shown. Select the vertex point shown. Note You may have to rotate the view to better identify the point. spse01540 Modeling assemblies 3-19

100 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships For the target, select the vertex point shown Modeling assemblies spse01540

101 More Assembly Relationships Create an Axial Align relationship Use the Axial Align relationship for the second relationship. Click the Axial Align relationship. Select the linear edge shown. spse01540 Modeling assemblies 3-21

102 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships For the target, select the linear edge shown Modeling assemblies spse01540

103 More Assembly Relationships Position the lid using the Angle relationship Use the Angle relationship to position the lid. Once placed, the angular value can be modified to reposition the orientation of the lid. Select the Angle relationship. Select the face shown as the face to measure to. Click the face shown as the face to measure from. spse01540 Modeling assemblies 3-23

104 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships When prompted to click on a plane in which the angle measurement will lie, click the edge shown. Note The Angle measurement is established. Click the Select tool Modeling assemblies spse01540

105 More Assembly Relationships Edit the angle Edit the angle and the position of the lid will change. Press Ctrl+R on the keyboard to rotate the view to a right view. In PathFinder, select lid.par:2 and then, in the lower pane, select the Angle relationship. Note Variable names and angle values may differ from the picture shown. This is not a problem. On the Placement command bar, click the Angle Format list, and then move the cursor over the eight options. Notice the difference in how the angle is measured in each of the different options. Click the Angle format which gives the measurement shown below. Change the angle to 90. spse01540 Modeling assemblies 3-25

106 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Change the angle to different values and observe the behavior. Change the angle to 190. On the ribbon, choose Tools tab Variables to display the Variable Table. Notice this angular value is shown here and can be edited from the Variable Table. Also the angular value can be driven via a formula to other values within the table. This completes the activity. Close the assembly document without saving Modeling assemblies spse01540

107 More Assembly Relationships Summary In this activity you learned to use the Angle relationship to position a lid, and modify the value of the angle to change the position of the lid. This activity is complete. spse01540 Modeling assemblies 3-27

108 Lesson Lesson 3: 3: More More Assembly Assembly Relationships Relationships Lesson review Answer the following questions: 1. Give an example of why a connect relationship would be used to position a part rather than mate or planar align relationship. 2. Give some examples of valid geometry that can be used to create a connect relationship. 3. Give some examples of connect relationship combinations Modeling assemblies spse01540

109 More Assembly Relationships Lesson summary In this lesson you learned to use the Connect relationship to position a lid using points, and to position a knob by connecting sphere centers together. spse01540 Modeling assemblies 3-29

110

111 Lesson 4: The Assemble command The Assemble command is an alternative method of positioning multiple parts that have been added to an assembly but not positioned in the assembly. Utilizing FlashFit techniques, the Assemble command allows changing parts with a right mouse click. spse01540 Modeling assemblies 4-1

112 Lesson Lesson 4: 4: The Assemble The Assemble command command Assemble command The Assemble command positions parts in an assembly. You can use this command to position a single part, or you can use this command to position several parts relative to each other without fully constraining each part in an ordered sequence. This type of workflow can make it easier to position a set of interrelated parts, such as when building a mechanism. After dragging a set of parts into an assembly, you can use the Assemble command to apply relationships between one of the parts and one or more target parts. To position a different part, click the right mouse button. To position a series of parts using the Assemble command, you first drag the set of parts into the assembly using the Parts Library tab. If it is a new assembly, the first part is automatically grounded. When you drag and drop the second part into the assembly, the Assemble command bar is displayed, but you can continue to drag parts into the assembly without positioning them. After the set of parts is placed in the assembly, you can use the Assemble command to position the parts. When you click the Assemble command, the Assemble command bar is displayed. You can use the FlashFit option to apply a mate, planar align, or axial align relationship, or choose from the complete set of ordered relationships. After you apply a relationship between two parts, the first part you select (A) remains selected so you can apply additional relationships to the part. 4-2 Modeling assemblies spse01540

113 The Assemble command To position a different part, click the right mouse button. You can then select a different part (A) and apply the relationships you want. The Assemble command is tightly integrated with the FlashFit positioning option. When you click the Assemble command, FlashFit is the default option. For more information on FlashFit, see the Assembly Relationships topic. Assemble command behavior Actions within the assemble command: FlashFit is the default assembly relationship creation mode and should be used. Once you select a part to position, it will become transparent. Once it is fully positioned, or another part is selected, it will no longer be transparent. If, in the middle of positioning a part, you decide to position another part, right-click to release the current part. It will no longer be transparent. The next part you select will then become transparent. If you work in wireframe, rather than shaded, you will not have the visual benefit of the selected part being transparent. For that reason, it is suggested that you use Shaded with Visible Edges display mode while using the Assemble command. Once a part is selected, it can be dragged to a new position with the left mouse button. The selected part is the part you are applying relationships to. Right-click to release the part. To rotate a selected part that is unconstrained, use CTRL + left mouse button. FlashFit will determine whether to use a Mate or Planar Align relationship based on the closest orientation of the faces being matched. It is good practice to rotate the selected part into the approximate position before selecting the faces. After FlashFit, if the faces are 180 out of position, click the Flip button on the command bar. Matching circular edges will quickly position a part, such as a fastener, in one operation. The axes are superimposed and the rotation is locked. You can unlock the rotation by editing the relationships in Assembly PathFinder. Refer to the section of this activity that addresses editing and error recovery. spse01540 Modeling assemblies 4-3

114 Lesson Lesson 4: 4: The Assemble The Assemble command command Activity: Using the Assemble command Overview The objective of this activity is to understand how to position parts using the Assemble command. Activity In this activity you will learn how to use the Assemble command. 4-4 Modeling assemblies spse01540

115 The Assemble command Overview When you complete this activity, you will be able to position parts in an assembly using the Assemble command. This activity teaches how to use the Assemble command to manipulate and fully position parts in an assembly. Objectives The activity covers the following: Settings that affect the Assemble command Manipulation and positioning of parts using the Assemble command Editing and error recovery Note Positioning parts with the Assemble command: There are many ways to correctly assemble the parts and subassembly associated with this activity. You will not be given specific instructions on how to assemble these parts other than the order in which to assemble the parts. How a part is positioned using FlashFit is predictable. With the Assemble command however, parts can be positioned incorrectly or over constrained. This activity will purposely position a part incorrectly so that the steps to correct the positioning will be covered. The rules on the behavior of the Assemble command are listed next. You will be instructed to use these rules where appropriate. spse01540 Modeling assemblies 4-5

116 Lesson Lesson 4: 4: The Assemble The Assemble command command Note Assemble command guidelines The following guidelines are used in positioning the parts in this assembly using the Assemble command. In the assembly you will be working with valve_housing.par which was placed first and is grounded. The other parts will be positioned relative to this previously positioned part. FlashFit is the default assembly relationship creation mode and should be used. Once you select a part to position, it will become transparent. Once it is fully positioned, or another part is selected, it will no longer be transparent. If, in the middle of positioning a part, you decide to position another part, right-click to release the current part. It will no longer be transparent. The next part you select will then become transparent. If you work in wireframe, rather than shaded, you will not have the visual benefit of the selected part being transparent. For that reason, it is suggested that you use Shaded with Visible Edges display mode while using the Assemble command. Once a part is selected, it can be dragged to a new position with the left mouse button. The selected part is the part you are applying relationships to. Right-click to release the part. To rotate a selected part that is unconstrained, use CTRL + left mouse button. FlashFit will determine whether to use a Mate or Planar Align relationship based on the closest orientation of the faces being matched. It is good practice to rotate the selected part into the approximate position before selecting the faces. After FlashFit, if the faces are 180 out of position, click the Flip button on the command bar. Matching circular edges will quickly position a part, such as a fastener, in one operation. The axes are superimposed and the rotation is locked. You can unlock the rotation by editing the relationships in Assembly PathFinder. Refer to the section of this activity that addresses editing and error recovery. 4-6 Modeling assemblies spse01540

117 The Assemble command Assemble command setup Open assemble.asm. Choose the Home tab->assemble group->assemble command. Click the Options button on the command bar. Set the options shown below, then click OK. Note The behavior of positioning faces with FlashFit will first be shown. For other parts, edges will be used. spse01540 Modeling assemblies 4-7

118 Lesson Lesson 4: 4: The Assemble The Assemble command command Assemble the parts beginning with the top cap Move the parts to their approximate final position. Select a part to move. The part will become transparent. With the left mouse button, drag the part to the position shown. Right-click to release the part and left-click to select a different part to drag. Position all the parts approximately as shown. Right-click to release the last part selected. Select the top cap. Zoom in on the top face of the valve housing. Using FlashFit, mate the bottom face of the top cap to the top face of the valve housing as shown. 4-8 Modeling assemblies spse01540

119 The Assemble command Select the cylindrical axis of a hole on the top cap, and then select the cylindrical axis of a hole in the top of the valve housing, as shown. To completely position the part, repeat the previous step beginning with a different cylindrical axis in the top cap, and a corresponding cylindrical axis in the valve housing. Once the part is completely positioned, it will become shaded and no longer be transparent. spse01540 Modeling assemblies 4-9

120 Lesson Lesson 4: 4: The Assemble The Assemble command command Position the first fasteners on the top cap Position the first fastener on the top cap. To begin positioning the next part, select the face shown of one of the fasteners. Select the face of the top cap as shown Modeling assemblies spse01540

121 The Assemble command FlashFit determines whether to apply a Mate or Planar Align relationship based on the orientation of each of the faces. If the fastener is placed reversed, as shown, click Flip on the command bar to correct. spse01540 Modeling assemblies 4-11

122 Lesson Lesson 4: 4: The Assemble The Assemble command command Select the cylindrical shaft of the fastener and the cylindrical axis of the corresponding hole. The fastener is positioned in the hole, but is transparent because there is freedom in the axis defined by the center of the shaft Modeling assemblies spse01540

123 The Assemble command Select the flat face on the head of the fastener as shown, and then select the face on the top cap as shown. The bolt rotates such that the planes become parallel and a floating offset is applied which locks the rotation of the bolt. spse01540 Modeling assemblies 4-13

124 Lesson Lesson 4: 4: The Assemble The Assemble command command Position the other fasteners using edge selection You will now position other fasteners by using FlashFit and selecting circular edges. Click the options button on the command bar and set the options as shown Modeling assemblies spse01540

125 The Assemble command Position the fastener using the edges shown below. Note Positioning by matching circular edges completely constrains the part by fixing the rotation. This is the preferred method. spse01540 Modeling assemblies 4-15

126 Lesson Lesson 4: 4: The Assemble The Assemble command command If the fastener becomes oriented as shown, it is because the original orientation of the faces of the fastener was closer to a Planar Align relationship rather than a Mate relationship. Note Because the part is completely constrained, the Assemble command has released this fastener and is ready to position another part. The fastener has become shaded indicating it is fully positioned. To position this fastener correctly, you will need to temporarily exit the Assemble command by clicking the Select Tool. Once the fastener is positioned correctly, click the Assemble command to continue positioning parts. If the fastener was placed upside down, select the fastener. It will become transparent. Select the Mate relationship, click Flip, then click OK to correctly position the fastener. To position the remaining two fasteners, use these steps. Click the Assemble command and select one of the remaining fasteners. To rotate the fastener into the approximate vertical position, click and hold CTRL while you left-click and then drag Modeling assemblies spse01540

127 The Assemble command Position the fastener by selecting the same circular edges as the previous part. The fastener will be oriented correctly because the orientation was close to the final position. Right-click to clear the selection when done. spse01540 Modeling assemblies 4-17

128 Lesson Lesson 4: 4: The Assemble The Assemble command command Position the handle subassembly You will now position the handle subassembly by using FlashFit and selecting circular edges. Position the subassembly handle and ball.asm by selecting the circular edges as shown Modeling assemblies spse01540

129 The Assemble command Use the Assemble command and the techniques learned from the previous steps to position each endcap into the correct position on the valve housing. This completes this activity. Close the assembly document. spse01540 Modeling assemblies 4-19

130 Lesson Lesson 4: 4: The Assemble The Assemble command command Summary In this activity you learned how to use the Assemble command to quickly assemble a group of parts into an assembly. If all the parts making up an assembly are placed in an assembly window, the Assemble command can be used to complete the positioning of the parts into the final assembly. This completes the activity Modeling assemblies spse01540

131 The Assemble command Lesson review Answer the following questions: 1. How do you move an unconstrained assembly component when using the assemble command? 2. How do you rotate an unconstrained assembly component when using the assemble command? 3. How do you select a different assembly component to position without exiting the assembly command? spse01540 Modeling assemblies 4-21

132 Lesson Lesson 4: 4: The Assemble The Assemble command command Lesson summary In this lesson you learned how to use the Assemble command to quickly assemble a group of parts into an assembly. If all the parts making up an assembly are placed in an assembly window, the Assemble command can be used to complete the positioning of the parts into the final assembly Modeling assemblies spse01540

133 Lesson 5: Designing in the context of an assembly When designing in the context of an assembly, you can construct the parts with either ordered or synchronous geometry based on which is appropriate for the desired outcome. In the activity, you will experience designing parts in context of a top level assembly using the tools provided. spse01540 Modeling assemblies 5-1

134 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Activity: Designing in the context of a Synchronous assembly Overview The objective of this activity is to explore designing in the context of an assembly with Solid Edge Synchronous technology. You will open an existing assembly and use adjacent parts to refine the sizing and spacing of the faces and parts in the assembly. You will also use geometry from one part to create a cavity in an adjacent part. Activity In this activity you will learn how Synchronous technology can be of benefit when designing in the context of an assembly. 5-2 Modeling assemblies spse01540

135 Designing in the context of an assembly Overview In this activity, you will modify parts in the context of the assembly using Solid Edge. spse01540 Modeling assemblies 5-3

136 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Open the assembly Open spindle_cover.asm. Activate all the parts. Note Click the Select command and click on each part in PathFinder. Each relationship that has been used to position the assembly can be viewed by moving the cursor over the relationships in the lower pane of PathFinder. These existing assembly relationships as well as Design Intent relationships are honored when manipulating geometry with Solid Edge. 5-4 Modeling assemblies spse01540

137 Designing in the context of an assembly Modify the plastic part to make the brackets fit The brackets holding the axle do not fit correctly on the plastic cylindrical part, and the face of the plastic part that the brackets attach to is not wide enough to accommodate the brackets. You will modify the parts in the context of the assembly to correct these problems. Set the Selection Priority to Face. Select the face shown with the steering wheel in the position shown. spse01540 Modeling assemblies 5-5

138 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Select the additional faces shown. You should have a total of 4 faces selected. 5-6 Modeling assemblies spse01540

139 Designing in the context of an assembly Select the axis of the steering wheel as shown. On the QuickBar, select the circle center key point. spse01540 Modeling assemblies 5-7

140 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Click the circular center of the end face of the axle. The 4 faces will move. Note Because symmetry about the base reference planes is preserved using the Design Intent panel options, the parts are modified on the opposite side as well. Clear the Selection. 5-8 Modeling assemblies spse01540

141 Designing in the context of an assembly Shorten the brackets Because the brackets are too tall, the axle is too far out from the plastic housing. You will shorten the bracket. Select the face and the cylinder shown. Move the origin of the steering wheel to the face shown. Note The steering wheel can be relocated by dragging the origin knob which is the large sphere at the center. spse01540 Modeling assemblies 5-9

142 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Drag the primary axis on the steering wheel so that the bracket becomes shorter. Enter mm. The axial alignment between the bracket and the axle force the axle to stay aligned with the hole in the bracket Modeling assemblies spse01540

143 Designing in the context of an assembly Note The axle moves with the bracket because of the Axial Align relationship used to place the axle. Clear the Selection. spse01540 Modeling assemblies 5-11

144 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Create clearance between the bracket and plastic housing The face of the plastic part is too close to the bracket. You will move the face inward. Select the face shown. Rotate the view to a right view and move the face somewhere between the bracket face and the next face on the shaft. Exact placement is not important. Because the part is symmetrical about the base, the design intent relationships built into the model are preserved using the Design Intent panel. These settings control the behavior such that the opposite face is also positioned correctly Modeling assemblies spse01540

145 Designing in the context of an assembly In-place activate the plastic part and create Inter-Part geometry for cutting the part After in-place activating the plastic part, inter-part faces and an inter-part body will be created from other parts in the assembly. spse01540 Modeling assemblies 5-13

146 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Clear the select set. Set the selection criteria to Part. Double-click the plastic part to in-place activate the part. You are now in the part environment but can still see the other parts in the assembly. Note Using Inter-Part Copy, you will copy needed geometry from the assembly. You need two planar faces to create bolt holes in the plastic part to attach the brackets. You will also need the body of beltdrive.par Modeling assemblies spse01540

147 Designing in the context of an assembly Click the Inter-Part Copy command. Note Linked Inter-Part copies of surfaces can only be created in the ordered environment. The Inter-Part surface created for this exercise does not need to be linked and we will stay in the Synchronous environment for this operation. Select the bracket. spse01540 Modeling assemblies 5-15

148 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly In the Select Faces step in the command bar, select Face. Select the face shown. Accept and then click Finish. Repeat for the opposite side Modeling assemblies spse01540

149 Designing in the context of an assembly Click the Inter-Part Copy command and select the part shown. spse01540 Modeling assemblies 5-17

150 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly In the Select Faces step in the command bar, select Body. Select the whole body shown. Accept the body, then click Finish. The body is created Modeling assemblies spse01540

151 Designing in the context of an assembly Cut the plastic part using the Inter-Part faces The two Inter-Part faces and the Inter-Part body, and a cutout will be used to cut the plastic part. Click the View tab and in the Show group, click Hide Previous Level. This will turn off the display of the other parts in the assembly Click the Sketching tab. Lock the sketch plane to the face containing the Inter-Part copies. Click Project to Sketch and select each of the 4 holes on the two Inter-Part faces. Hide the Inter-Part Copy faces, used to create the holes, in PathFinder. Click the Extrude command. Create cutouts from each of the holes. spse01540 Modeling assemblies 5-19

152 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly Now you will draw a sketch for the first cutout in the housing. Select the sketch plane shown Modeling assemblies spse01540

153 Designing in the context of an assembly Draw the sketch below and create an open cutout that extends the full length of the part. Note In the Relate group on the ribbon, use the Equal relationship to make the lines the same length. The angle between the lines is 120 o. Use the Horizontal/Vertical relationship to line up the ends of the lines vertically. Intellisketch may put a Perpendicular relationship at the intersection of the two lines. You will need to delete that relationship in order to get the 120 o driving dimension placed. spse01540 Modeling assemblies 5-21

154 Lesson Lesson 5: 5: Designing Designing in theincontext context of anof assembly an assembly The part is shown. Click the Surfacing tab. In the Surfaces group, click the Offset command Modeling assemblies spse01540

155 Designing in the context of an assembly In the Select step in the command bar, set Select to Body. Select the Inter-Part Copy shown and Accept. spse01540 Modeling assemblies 5-23